CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

time-averaged specific variables as sources

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 5, 2017, 11:28
Default time-averaged specific variables as sources
  #1
Member
 
Join Date: Jun 2017
Posts: 40
Rep Power: 8
cardioCFD is on a distinguished road
Hi,

I am trying to simulate a chemical reaction with a kinetic rate depending on the "time averaged shear rate" at each point. The simulation is transient and periodic.

As an initialisation, I ran the simulation (only flow) for one period calculating transient statistics (Trnavg) for shear rate.

In the main simulation, I used the previous flow-only simulation as initial values and tried to access ShearRate.Trnavg in a source (subdomain) that defines the reaction, but I get the GETSOU error in the solver.

Note: ShearRate is an algebraic equation variable with values equal to Shear Strain Rate at each point.

Note: I can use ShearRate.Trnavg on the boundaries, the only problem is that I cannot call ShearRate.Trnavg in the source.

Any comment is highly appreciated. Thanks.
cardioCFD is offline   Reply With Quote

Old   June 5, 2017, 14:45
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 1,799
Rep Power: 31
Opaque will become famous soon enough
Would you mind posting the error message you got ?

I understand you setup the case as:

Domain level AV definition:
MyAVTrnavg = Shear Strain Rate.Trnavg

Subdomain level source definition

Source = Function (MyAVTrnavg)

correct ?
Opaque is offline   Reply With Quote

Old   June 6, 2017, 03:06
Default
  #3
Member
 
Join Date: Jun 2017
Posts: 40
Rep Power: 8
cardioCFD is on a distinguished road
Hi,

Thank you for your message. Here is the error:

================================================== ====================
TIME STEP = 101 SIMULATION TIME = 8.8741E-01 CPU SECONDS = 1.134E+05
(THIS RUN: 1 4.4150E-03 3.463E+02)
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 3.463E+02
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom | 2.97 | 2.3E-04 | 1.9E-02 | 4.4E-02 OK|
| V-Mom | 1.96 | 1.4E-04 | 1.1E-02 | 8.2E-02 OK|
| W-Mom | 1.29 | 8.8E-05 | 5.8E-03 | 1.2E-01 ok|
| P-Mass | 3.63 | 1.2E-04 | 1.7E-02 | 9.9 9.6E-02 OK|
+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Failed to calculate sources in GETSOU for RESSRC_A from director- |
| y "" on location "sources". Error return code is: OPER |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine GETSOU |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

For now, I created another volumetric/algebraic equation variable called TASR in both initialisation and the main simulations, this variable is nothing but ShearRate.Trnavg. Now I can access this new variable in defining sources and it seems to work for now. I would appreciate any further comment on that.

Thanks a lot.
cardioCFD is offline   Reply With Quote

Old   June 6, 2017, 09:22
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,799
Rep Power: 31
Opaque will become famous soon enough
Unfortunately, that is the workaround approach.

From the message, the function GETSOU says it has an error handling the OPER attribute.

Shear Strain Rate.Trnavg is a combination of Variable.Operator, so it can be assumed it could not process the ".Trnavg" part.

By copying into an algebraic variable, you have bypassed the handling of the ".Trnavg"..

You should be good to go.
Opaque is offline   Reply With Quote

Old   July 30, 2018, 07:55
Default
  #5
New Member
 
Sascha
Join Date: May 2012
Location: Germany
Posts: 14
Rep Power: 13
SaschaGH is on a distinguished road
Thanks Opaque for the explanation, just helped me a lot!
Best
SaschaGH is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Elastic or Plastic Deformations in OpenFOAM NickolasPl OpenFOAM Pre-Processing 36 September 23, 2023 08:22
How to export time series of variables for one point? mary mor OpenFOAM Post-Processing 8 July 19, 2017 10:54
Compression stoke is giving higher pressure than calculated nickjuana CFX 62 May 19, 2015 13:32
plot over time fferroni OpenFOAM Post-Processing 7 June 8, 2012 07:56
Constant velocity of the material Sas CFX 15 July 13, 2010 08:56


All times are GMT -4. The time now is 13:05.